CNC Tooling

[techhelpbb]

Originally Posted by sanddrag

I evaluated BobCAD/CAM (along with half a dozen others) and I can't say I'd recommend it based on my 2 hour demo of it. The UI and workflow seems primitive and complex compared to some other software packages. Also, once contact is initiated, be prepared to deal with their relentless sales force. You're basically on their contact list for life at that point, and you'll hear from them at least twice a month.

BobCAD is extremely aggressive about sales.
A bit too aggressive at times.

I find there interface a bit old fashioned in visual style but I have found that depending on your perspective of the CAD/CAM/CNC workflow BobCAD can be great product. I own a few versions with and without dongles.

There is unfortunately a learning curve.
I had the same trouble the first time I used it.
Once I got the hang of it things went smoother.
I could never have made due with a 2 hour demo either.

Originally Posted by Mr. Mike

• When it comes to cutting aluminum, stay away from any coatings that are gray to black. They are TiAlN (Titanium Aluminum Nitride), AlTiN (Aluminum Titanium Nitride), and TiAlSiN (Titanium Aluminum Silicon Nitride). Aluminum will stick and nasty thing will happen.

Does this not depend on the speed of the spindle?

Usually you have to spin the TiAlN end mills at higher speeds to make the coating operate as intended (18k to 22k RPM).
You would not want to use a TiAlN end mill too slowly or it will be worse than an HSS end mill.

Then there's the other issue, the higher the spindle speed the higher the IPM you need to move or risk rubbing. Not a problem for good machines but a problem for light weight gantry mills.


Generally and not in reply to anyone:
I linked this in a topic in the motor section but I will link it here as well:
http://blog.cnccookbook.com/2012/03/...tting-success/
Props to scottandme for posting a reference to G-Wizard as well (last page).

The issue I have with this topic is that I suspect that the different teams have different CNC machines.
A servo driven bridge or turret mill will have different requirements than a stepper driven gantry mill.
The bridge or turret has greater rigidity.
Depending on the spindle operating range it will impact the IPM.

It is hard to pick out what machine is what.
Some of the machines might be using steppers and therefore must target lower IPM feeds.
Some of the machines might have less cooling.
Some of the machines might have higher speed spindles with no ability to go slower.
The key elements that make this work depend on the knowing the machine sore spots.

For example:

Originally Posted by sanddrag

On our router at ~20,000 RPM, we've had a lot of trouble cutting aluminum with a standard 1/4" 3 flute carbide variable helix endmill we use with great results at 6,000 RPM with coolant on the mill. On the router, it just wants to load up and melt/weld chips. I'm thinking a 2-flute would give better chip evacuation.

Currently, our coolant system on the router is a student and a spray bottle of WD40.

I assume the mill in question is a turret type like a Bridgeport?

At this link...
http://www.daycounter.com/Calculator...lculator.phtml

Plug in 0.25", 300SFM, 3 flutes.
You get: about 4,500 RPM, 27.5 IPM
Makes sense that this works.

Plug in 0.25", 1,310SFM, 3 flutes
You get: about 20kRPM, about 120 IPM
This is probably not going to work.
I would be a bit suspicious of a carbide end mill rated at 1,310SFM uncoated.
Even more suspicious if your router can sustain the feed rate to keep it from rubbing.

At a spindle speed of 20kRPM I think you should consider a TiAlN end mill for the router with 2 flutes and 1/8" diameter.
That would get you:
655SFM, 20kRPM spindle speed, 80IPM feed.
If your gantry mill is outfitted with either really powerful steppers or servos it will work.

Try this:
http://www.wttool.com/index/page/cat...lls+%28USA%29/

Otherwise if you can't get the power from the steppers on your gantry:
Use a single flute as others have suggested and you'll divide that feed rate in half.
At that point if it's not enough edit your depth of cut and tool path to accommodate.